Designfusion Blog

NX Emboss Body Feature

Stephen Rose - Tuesday, August 11, 2015

Overview

An often overlooked feature in NX is the Emboss Body. The Emboss Body can simplify the process when designing a part that may need to be adjusted to suit
surrounding parts—a process which would otherwise require multiple steps and the use of several unite, trim, and subtract commands to accomplish
the same design goal.

The power of the Emboss Body is not only the simple ability to impress the shape of another body into the part you are designing, but also the complex
ability to specify offsets and thicknesses to rebuild the wall-stock of the part being embossed.

Where to find it

The Emboss Body can be found several ways. If you are familiar with the traditional NX menu you will easily find it under Menu->Insert->Combine->Emboss
Body

If you are more comfortable with the NX Ribbon style interface first you will need to have the Advance Role loaded, or your own customized Role where you
have already added the Emboss Body to your ribbon. Then you will find it in HOME->Feature Group MORE->Combine Group->Emboss Body.

There is always the command finder where you can search the Emboss Body feature and access it directly.

Use

Here we have a simple (yellow) molded part developed using the shell command with structural ribs and boss feature added.

Now in this example the assembly this part belongs to has another part (shown grey) that interferes. (See grey dome protruding through into back side of
boss, rib and wall-stock in picture below). So we need to remodel our (yellow) part to accommodate this body. Traditional modeling techniques of modifying
the (yellow) part involved building surfaces from the intruding part, offsetting for clearance, building new wall-stock then stitching surfaces or
doing Boolean operations on all these to get back into one body. The Emboss Body handles all this for us.

Now let’s take a closer look at the interference using our Clipping Section Editor (Ctrl-H). Setting the clipping plane through the boss center we can
see how the interfering part intrudes into our (yellow) part. Also note in this example we’ve set the two options for better clarity. Under the CAP
settings we’ve turned on Show Cap and also turned on the Show interference and set the interference colour to Red. We’ve also turned on the Section
Curve preview settings and set the section colour to Black to contrast the wall-stock. With the interference setting and section curves set it gives
us a clearer indication of the interference that is happening.

We now enter the Emboss Body via the Menu or Ribbon Bar method.

We select our (yellow) part as the target, and the (grey) interfering body as the tool. With the Thicken option unchecked, and the tool clearance offset
set at 0, the results we get are similar to a simple Boolean subtraction. Note: This is not how we want to develop our final part. This is just to
illustrate how the options work and the differing output achieved.

In order to get our part constructed without the void that the previous views showed we need to check the Thicken option and set the value to the wall-stock
that we want created. We also want to set a clearance offset zone so that the parts don’t contact each other.

With a couple of finishing radii and fillets the part is now complete with clearance to the intruding part and proper adjustments to the wall-stock at
the ribs and boss features.

If you would like to learn more about this operation and other advanced operations, you should attend one of our advanced NX CAD courses. To arrange for
advanced training please contact your Account Manager, or contact us directly at[email protected].